Printed wiring board having impedance-matched differential pair signal traces

ABSTRACT

A printed wiring board having differential pair signal traces has increased spacing between signal-carrying vias and ground or power planes and/or is equipped with selectively placed ground vias to enhance the impedance matching of the signal traces.

CROSS-REFERENCE TO RELATED APPLICATION

This application is a division of U.S. patent application Ser. No.10/356,660 entitled “Impedance Matching of Differential Pair SignalTraces on Printed Wiring Boards” filed on Jan. 31, 2003, the disclosureof which is hereby incorporated in its entirety by reference.

BACKGROUND OF THE INVENTION

1. Field of the Invention

This invention relates to printed wiring boards (PWB's) also referred toas printed circuit boards (PCB's) when populated with components. Moreparticularly, it relates to printed wiring boards having differentialpair signal traces.

2. Description of the Problem and the Related Art

In digital circuits, it is common to represent a binary “zero” with onevoltage level and a binary “one” with another, different voltage level.By way of example, a logical “one” might be represented by a +5 voltsignal level and a logical “zero” by 0 volts on a given signal line.Inasmuch as voltages are relative, it is common to reference the signallevel to ground. Signals formed in this way are referred to assingle-ended signals.

One disadvantage of this scheme is that the noise margin, or levelbetween the guaranteed zero and one levels, is relatively small. It ispreferable—i.e., more definite—to have a large noise margin. This isespecially true at high frequencies where settling times can berelatively long due to ringing and other high frequency components offast-rise signals.

The above-described disadvantage can be avoided by the use ofdifferential pair signal transmission means. In this way, the signalstate is not referenced from either ground or a high level but is basedon the voltage difference between the two signals being above a givenlevel. One representative case is shown in FIG. 1 wherein differentialpair AB is comprised of Line A and Line B which may be at 0 or +5 vdc. Alogical zero is represented by Line B being high—e.g., about +5 vdc—andline A being low—e.g., about 0 vdc. A logical one is represented by LineA being high and Line B being low. This scheme approximately doubles thenoise margin as compared to single-ended cases.

Printed wiring boards (PWB's) or printed circuit boards (PCB's) may havesignal lines comprised of traces on the top, bottom and/or interiorlayers of the board.

Signal wires (traces) on the printed wiring board carry signals betweenmodules and between modules and input/output connections to the wiringboard. In some circumstances, it is necessary for the signal lines to berouted on different layers in a PWB. “Vias” or via service terminals(VST's) are used to perform this layer-to-layer connection.

Vias may be “blind” holes which are open to one surface of the wiringboard but do not extend to the opposite surface; they may be “buried”holes which connect only internal layers of the board and do not extendto either surface of the printed wiring board; or they may be platedthrough-holes which extend the full thickness of the board and open tosolder pads on both surfaces of the board.

Conventional routing of differential pair signal lines on or withinPWB's can result in bandwidth limitations for the signals due toimpedance mismatches. This is particularly the case for high speedcircuits—for example those running at 1 gigahertz and above. Any sourceof impedance mismatch becomes of greater concern as frequencies increasebecause of increased distortion of the waveforms in data transmissionlines, resulting in poor eye patterns, jitters, overshoot, ringing, slowrise/fall time, etc. Furthermore, the impedance mismatch increaseselectromagnetic interference (EMI). Thus, any technique which reducesimpedance mismatch for a reasonable cost is desirable.

BRIEF DESCRIPTION OF THE DRAWINGS

FIG. 1 is an illustration of voltage levels on a differential pair ofsignal traces.

FIG. 2 is cross sectional view of a printed wiring board of the priorart.

FIG. 3 is a top plan view of selected layers of a printed wiring boardhaving one embodiment of the invention.

FIG. 4 a is a cross sectional view of a printed wiring board of theprior art.

FIG. 4 b is a cross sectional view of the same printed wiring boardwhich incorporates one aspect of the present invention.

FIG. 5 is a top plan view of a portion of a printed wiring board havingone embodiment of the invention.

DETAILED DESCRIPTION OF THE INVENTION

A typical, multi-layer printed wiring board 10 with signal layers andground layers is shown in cross section in FIG. 2 wherein a driver and areceiver are connected by way of signal path 12. Signal wires (traces)on the printed wiring board carry signals between modules and betweenmodules and input/output connections to the circuit board. Alsoillustrated in FIG. 2 is the phenomenon of pad-to-ground capacitance.Two electrical conductors in proximity to each other will exhibit acapacitance between them. In general, the capacitance will increase withdecreasing distance of separation. The impedance of signal traces can beaffected by the proximity of such signal traces to ground planes in aprinted wiring board. At higher signal frequencies (e.g., greater thanabout 1 Gigahertz), the capacitance between signal lines and ground maysignificantly impact the impedance of the signal trace. It will beappreciated that at gigahertz frequencies, power planes in a printedwiring board can produce the same effect—i.e., the capacitance between asignal trace and a power layer in the PWB can adversely affect theimpedance of the signal trace. Power planes and ground planes in a PWBmay be considered “voltage planes” inasmuch as they are typicallymaintained at relatively constant potentials.

It has been found that the vias used to transfer differential pairsignals between layers of a PWB can be a source of impedance mismatch.It has also been found that the impedance matching of differential pairsignals comprised of two signal traces on a PWB which include vias tochange routing layers can be improved by increasing the spacing toground planes and/or providing a special ground via proximate the twovias of the differential pair traces. It is believed that thisadditional ground via provides a current return path for the signalalong the PWB thickness direction and favorably alters the dimensions ofthe electromagnetic ground plane. The impedance of a line can bemeasured, for example, by Time Domain Reflectometry (TDR). Thus, theefficacy of the method disclosed herein can be quantified and theplacement of one or more ground vias on the PWB may be optimized so asto provide the best possible impedance matching of the differential pairtraces.

FIG. 3 is a top plan view of a multi-layer PWB employing one embodimentof the present invention. The PWB comprises traces 14 and 16 forming adifferential pair signal line AB. The differential pair signal lines areshown in partial perspective as they traverse an interior layer of thePWB and electrically connect with signal vias 18 in order to reach anexterior surface of the PWB and connect to signal pads 22 by means oftop layer signal traces 20.

FIG. 4 a is a cross-sectional view of a conventional 12-layer printedwiring board in the vicinity of a via 18 which comprises a portion ofthe signal path 12. Stubs 26 provide electrical continuity to test pointaccess pads 28 which may be contacted by test equipment probes in orderto sample the signal. Of particular note are non-functional pads 30attached to via 18 in certain signal layers of the PWB and the viaground/power plane clearance which is typically about 32 mils.Non-functional pads may be an artifact of the CAD layout library used toproduce the PWB which typically incorporate a pad of specific size atsignal layers penetrated by a via service terminal.

FIG. 4 b is a cross-sectional view of the same PWB as depicted in FIG. 4a which has been modified in accordance with certain aspects of thepresent invention, namely the elimination of non-functional pads incertain signal layers and an increase in the via ground/power planeclearance to approximately 60 mils. This increased spacing has beenfound to decrease the trace-to-ground plane capacitance so that noappreciable impedance mismatch occurs at those points.

In some instances it is difficult to match the impedances of adifferential pair of signal traces. It is often desired to maintain a50-ohm impedance in a signal trace. Changing the trace-to-ground planecapacitance by increasing the spacing between signal vias andsurrounding ground or power planes can affect the signal impedance. Anadditional aspect of the present invention is the addition of a groundvia to provide some ground reference and to maintain the impedance ofthe signal trace at about 50 ohms. Such additional ground vias may notbe necessary in those cases where the two lines of a differential pairsignal trace are nearly perfectly matched.

FIG. 5 shows ground plane layer 32 in PWB 10. Signal traces 14 and 16(shown in partial perspective as dashed lines) are in a different layerof PWB 10 and are in electrical contact with signal vias 18. A typicalspacing S between signal traces 14 and 16 which comprise a differentialpair signal trace is about 14 mils. A preferred radial spacing P betweensignal vias 18 and the surrounding ground conductor 32 in accordancewith the present invention is from about 54 to about 66 mils. Aparticularly preferred radial spacing P is about 60 mils. As shown inFIG. 5, the unplated circular regions surrounding signal vias 14 and 16may overlap one another so as to form a single 8-shaped unplated region34.

Also shown in FIG. 5 is signal ground via 24. Ground via 24 comprises aplated through-hole, which, in some embodiments may fill with solder. Itwill be noted that, in the embodiment illustrated, ground via 24 islocated approximately midway between linear extensions of signal traces14 and 16. It will be appreciated by those skilled in the art that thespacing between signal traces 14 and 16 need not be the same as thatbetween traces 20 on the exterior surface of PWB 10. In someembodiments, signal traces 14 and 16 may be curved rather than linear orincorporate curved segments so as to adjust the spacing between thetraces to match that of the signal vias 18.

In the embodiment illustrated, signal vias 18 as well as ground via 24are plated through-holes. In other embodiments, the signal vias and/orthe ground via may be blind vias, buried vias, or any combinationthereof.

In general, the signal ground via should be approximately the samelength as that of the signal trace vias of the differential pair—i.e.,the ground via should traverse the same number of layers and morepreferably the very same layers of the PWB traversed by the signal vias.The ground via may be in electrical contact with one or more groundplane layers in the PWB. As illustrated in FIGS. 3 and 5, the ground viamay be advantageously placed between linear extensions of signal lines14 and 16 (as well as signal traces 20 and equidistant from signal vias18 comprising the differential signal pair. It is preferable that thesignal ground via not have a non-functional pad. Typical routing layerchanges will minimize the stub length by changing the signal from uppersignal layers to lower signal layers or vice versa. If the PCB thicknessis 0.125 inch, the high speed differential pair traces routed throughthe PCB will have their impedance matched during the trace routingchange from one layer to another.

The optimum location of ground via(s) 24 on PWB 10 may be determinedempirically by time domain reflectometry to obtain the desired signalimpedance and to match the impedances of the lines comprising thedifferential pair signal trace. Computer simulations may also be used tooptimize the positioning of the ground via(s) in accordance with thepresent invention. As shown in FIG. 5, one particularly preferredconfiguration has been found to be equidistant spacing of the ground viaand the two associated signal trace vias with the ground via beinglocated on a line drawn midway between the two signal traces and on theside of the signal vias opposite to the interior-layer signal traces.

While the present invention has been described with respect to a limitednumber of embodiments, those skilled in the art will appreciate numerousmodifications and variations therefrom. It is intended that the appendedclaims cover all such modifications and variations as fall within thetrue spirit and scope of this present invention.

1. A multilayer printed wiring board comprising: a first pair of signaltraces on a first layer of the printed wiring board; a second pair ofsignal traces on a second layer of the printed wiring board; a groundplane on a third layer of the printed wiring board comprised of groundconductors; a power plane on a fourth layer of the printed wiring boardcomprised of power conductors; via service terminals connecting eachmember of the first pair of signal traces to a like member of the secondpair of signal traces which via service terminals traverse the groundplane and power plane and are radially spaced apart from the groundconductors and power conductors by about 60 mils.
 2. A multilayerprinted wiring board comprising: a first pair of signal traces on afirst interior layer of the printed wiring board; a second pair ofsignal traces on a second interior layer of the printed wiring board;blind via service terminals connecting each member of the first pair ofsignal traces to a like member of the second pair of signal traces; anda ground via service terminal for conducting the electrical currentwhich comprises the signal return said ground via service terminallocated approximately equidistant from and substantially parallel to thesignal trace via service terminals.
 3. A printed wiring board as recitedin claim 2 wherein the signal traces are differential pair signaltraces.
 4. A printed wiring board as recited in claim 2 wherein theground via service terminal and the via service terminals of the twosignal traces are substantially collinear.
 5. A printed wiring board asrecited in claim 2 wherein the ground via service terminal isapproximately the same distance from the signal trace via serviceterminals as the signal trace via service terminals are from each other.6. A multi-layer printed wiring board having a top surface, a bottomsurface and one or more interior layers which comprises: a first pair ofsignal traces on the top surface of the printed wiring board; a secondpair of signal traces on an interior layer of the printed wiring board;via service terminals electrically connecting each member of the firstpair of signal traces to the like member of the second pair of signaltraces; and, a ground via service terminal for conducting the signalreturn current which traverses the thickness of the printed wiring boardfrom the top surface to the bottom surface and which is proximate to andsubstantially equidistant from the via service terminals connecting eachmember of the first pair of signal traces to the like member of thesecond pair of signal traces.
 7. A printed wiring board as recited inclaim 6 wherein the via service terminals are plated through-holes inthe wiring board.
 8. A multilayer printed wiring board comprising: afirst pair of signal traces on a first layer of the printed wiringboard; a second pair of signal traces on a second layer of the printedwiring board; a ground plane on a third layer of the printed wiringboard comprised of ground conductors; a power plane on a fourth layer ofthe printed wiring board comprised of power conductors; via serviceterminals connecting each member of the first pair of signal traces to alike member of the second pair of signal traces which via serviceterminals traverse the ground plane and power plane and are radiallyspaced apart from the ground conductors and power conductors by about 60mils; and, a ground via service terminal for conducting the electricalcurrent which comprises the signal return said ground via serviceterminal located approximately equidistant from and substantiallyparallel to the signal trace via service terminals.
 9. A multilayerprinted wiring board comprising: a first pair of signal traces on afirst layer of the printed wiring board; a second pair of signal traceson a second layer of the printed wiring board; a voltage plane on athird layer of the printed wiring board comprised of electricallyconductive material; via service terminals connecting each member of thefirst pair of signal traces to a like member of the second pair ofsignal traces which via service terminals traverse the voltage plane andare radially spaced apart from the electrically conductive material onthe voltage plane by about 60 mils.